Thread processing methods in CNC machining: how to pick and run each one

• 1
  Key takeaways
• 2
  How the five thread processing methods in CNC machining differ
• 3
  Rigid tapping: fast, cheap, and unforgiving
• 4
  Thread milling: one tool, many diameters
• 5
  Single-point threading: the fallback for big and odd threads
• 6
  Thread rolling and forming: moving metal instead of cutting it
• 7
  How to run a threading job step by step
• 8
  Thread processing methods in CNC machining compared

Thread processing methods in CNC machining split into two families: those that remove material and those that move it. Tapping, thread milling, and single-point threading cut metal away. Thread rolling and thread forming push metal into shape. The family you pick decides the machine setup, the tool, and the hole size you drill first. It also decides whether the thread is stronger or weaker than the parent material.

Cutting methods need a drilled core hole that matches the thread's minor diameter. A cut M8 × 1.25 thread in aluminium starts from a 6.8 mm drill. Moving methods need a different core, because the material has to flow outward into the flanks. The same M8 × 1.25 hole for a forming tap starts from about 7.4 mm. Get that number wrong and the tap either snaps or leaves a loose thread.

Thread milling and single-point threading use a rotating tool that orbits a stationary or slowly rotating part. That means one tool can cut any diameter inside its working range. A single 10 mm thread mill covers M6 to M14 without a tool change. Tapping cannot do that. Each pitch and diameter needs its own tap, which is why a shop running many thread sizes keeps a large tap cabinet.

• 1
  Cutting toolsTaps, thread mills, and single-point tools remove chips.
• 2
  Forming toolsRoll taps, thread rolls, and forming taps displace metal.
• 3
  Core hole ruleForming needs a larger core hole than cutting for the same thread.

Rigid tapping is the default for holes from M1.6 to about M16 in a stable setup. The tap is held in a synchronized holder or a solid collet, and the spindle speed and feed are locked to the thread pitch. On a machine with rigid tapping, the Z axis reverses exactly in step with the spindle, so the tap enters and exits without a floating holder.

Speeds depend on material. In 6061 aluminium, run 300 to 600 rpm with a high-speed steel or carbide tap and plenty of cutting fluid. In 304 stainless, drop to 80 to 150 rpm and use a tapping paste or oil. In 4140 steel, 100 to 200 rpm is a safe starting range. A tap that squeals is running too fast or has too little lubrication.

The failure mode is almost always the same. Chips pack into the flutes, torque spikes, and the tap breaks in the hole. Blind holes make this worse because there is nowhere for the chip to go. Use a spiral-flute tap, which pulls chips up and out of the hole, and drill the core hole 1 to 2 mm deeper than the thread depth so the tap tip has clearance.

Bottoming taps reach closer to the floor of a blind hole but have almost no room for chips. If a blind hole needs thread to within 1 mm of the bottom, tap it in two passes: a spiral-flute tap first, then a bottoming tap. Never run a bottoming tap at production speed. Keep it under 150 rpm and peck the last few millimetres.

Thread milling uses a smaller single-form or multi-form cutter that helical-interpolates around the bore. The tool enters from the top or through the hole, orbits one full turn plus the lead-in and lead-out arcs, and exits. The thread form comes from the tool profile, not from the machine's Z-to-spindle sync. That is why thread milling works on machines without rigid tapping.

The main advantage is range. A thread mill with a 10 mm shank can cut M6 through M16 at the same pitch. It also cuts right- and left-hand threads with the same tool. For a shop that runs prototypes and low-volume work, one thread mill replaces a row of taps and cuts tool-change time.

Chip control is easier because the cut is interrupted and the chips are short. Blind holes are less risky too, since the tool can be programmed to stop short of the floor. But thread milling is slower per hole than tapping. On a 100-hole run of M6, tapping wins on cycle time every time. Use thread milling for large threads, thin walls, and one-off parts.

Rigidity still matters for thread milling. The cutter is small relative to the thread, so it deflects. Keep the radial depth of cut light, run a high spindle speed, and use climb milling so the tool pushes the chip out of the cut. A thread mill that chatters leaves a rough flank and a pitch diameter that drifts out of tolerance.

Single-point threading cuts one thread at a time with a sharp tool that follows a helical path. It is the oldest method on the list and still the most flexible. Lathes use it for shafts and fittings. Mills use it for bores that are too large or too unusual for a tap or a thread mill.

The clear use case is a thread that has no standard tool. A 1.75 mm pitch on a 40 mm bore, a left-hand buttress form, or a thread that must be cut to a measured pitch diameter all point to single-point work. The operator can measure the flank with a thread micrometer and adjust the tool offset without scrapping the part.

The trade-off is time and skill. A single-point pass needs several spring passes to hit the pitch diameter, and the tool wears quickly on the tip. Speeds run lower than thread milling for the same material. In 6061 aluminium, 200 to 400 rpm with a carbide insert is a reasonable start. In titanium, drop to 60 to 120 rpm and expect more passes.

Single-point threading also handles interrupted threads, such as a thread cut across a keyway or a cross-hole. A tap would catch and break on the interruption. A single-point tool just keeps following the helix. That makes it the only practical choice for some hydraulic and manifold fittings.

Thread rolling presses a hardened die against a rotating blank and squeezes the material into the thread form. No chips are produced. The grain flow follows the thread profile instead of being cut across it, so the thread is stronger in fatigue than a cut thread. Rolled threads are standard on bolts and studs for that reason.

On a CNC lathe, thread rolling needs a special attachment and a blank diameter that matches the pitch diameter, not the major diameter. Get the blank right and the die forms a full thread in a few seconds. Get it wrong and the die overloads or the thread comes out undersized. This is a high-volume method. It does not make sense for a 20-piece run.

Thread forming, also called cold forming or fluteless tapping, uses a lobed tap that displaces material in a drilled hole. There are no flutes, so no chips are generated. That is the main reason to choose it for blind holes in aluminium, brass, and copper, where a chip left in the hole can cause a loose fastener or a short circuit later.

Forming taps need more torque than cutting taps, so the machine must have enough spindle power and a rigid setup. The hole must be drilled to the correct forming core diameter, which is larger than the cutting core. In 6061 aluminium, an M6 × 1.0 forming tap needs about a 5.55 mm hole versus 5.0 mm for a cutting tap. Lubrication is critical because there is no chip to carry heat away.